| rtarbell |
One of the "new" features I just learned about in EagleLite is the hatched style ground plane (I always used a solid ground plane before).
Are there any advantages to using a hatched ground pland as opposed to a solid ground plane? I would think that the spaces in the hatched ground plane would be vulnerable for high frequency noise; why not just go solid? |
|
|
| I_Forgot |
It is easier to solder to a hatched ground plane because it doesn't suck away the heat from the joint so quickly.
I_F |
|
|
| pinkmouse |
| Hatched ground planes are a hangover from obsolete PCB manufacturing technologies and as such, not really needed any more. I_F's problem can be solved by using "thermals" where a little of the copper surrounding the pad is etched away. Eagle has a setting for this. |
|
|
| jcx |
the reason for hatched planes on a outer layer is to balance the amount of copper on each layer with respect to the midline of the of the board stackup, with a solid plane on one side and only a few traces on the other face a board can come out warpped due to the tce imbalance
DCR is higher with less copper but until hole dimensions approach the wavelength of the EMI frequency there is isn't much loss of effectiveness, obviously E field sheilding effectiveness is lowered by the hole area % |
|
|
| pinkmouse |
| quote: | Originally posted by jcx
...with a solid plane on one side and only a few traces on the other face a board can come out warpped due to the tce imbalance... |
As far as I understand it, it wasn't so much a problem in PCB manufacturing, but more a case that PCBs would distort if large ground planes were present when flow soldered. This was before the days of solder resist layers. So unless you like the look, I'd stick with solid. |
|
|
| jcx |
depends how big your board and how flat you need
stress is built in by high temp cure, copper and fr4 not matching in tce very well
for home build, mostly thru-hole or small smts it won't make much difference and solid gnd plane is fine |
|
|
| TwoSpoons |
| Hatching is still useful for homebrew pcb - by keeping the etch/non-etch copper density even across the pcb, undercutting of fine tracks is greatly reduced as the whole pcb tends to finish etching at the same time. Same applies to not leaving vast areas of open space - by the time it has etched away, your thin tracks will be very thin, or missing altogether. |
|
|
|
